NO Agreement between ProE and ANSYS

[msiva1981]

Hi,

I analysed a frame in Pro E and obtained Stresses and Deflections. I
imported the FEM Model to perform the same analysis in ANSYS (using
.ans file). The Von mises stresses i obtain using Pro E and ANSYS are
entirely different



Pro e

Min 0.1786psi

Max 90000 psi

ANSYS

Max 41236 psi

Min 18.904 psi



I have attached Jpeg files for your review. Let me know where things don't seem right

View attachment 4351


View attachment 4352

 

[misiek_wro]

Hi,

hmmm..., what diffrent is between deflection ? (can You attach the file?)

michal

 

[msiva1981]

Hi misiek_wro,
Thanks for the reply
Deflection is similar
ANSYS 0.28 in
Pro E 0.27 in
I have attached the pro E file and the .ans file from ANSYS
Siva

 

[msiva1981]

forgot to attach file. Here it is
2007-10-30_131932_Analysis_siva.zip2007-10-30_132455_Ansys_file_siva.zip

 

[burnsp]

Are you sure that all the material properties are the same, i.e. elastic modulus?

 

[msiva1981]

Hi Burnsp,
Thanks for the reply
I first did the Analysis on Pro E (Native mode). Used the FEM mode then to generate the .ans file, then solved it using ANSYS. So if i do not have to do anything special about the material properties, they should be the same.
Siva

 

[msiva1981]

I checked the Material properties. Its is 29e6 psi (young's Modulus of Steel)
Thanks
Siva

 

[burnsp]

As long asits the same for both Pro/E and Ansys. Sorry, I don't have any ANSYS experience.

 

[miya]

The ratio of your differing results is:


Pro/E / ANSYS = 90,000 / 41,236 = 2.18


so it is probably not a units issue since it is not a factor of 386.4 or 32.2 or 12.


Where does the peak stress occur in each model? Is it at a singularity location? e.g. the sharp corner where the top beam and the side columns meet in your Pro/E model?

 

[msiva1981]

Iam trying to figure that out. ANSYS lists results by nodes. Is there a way to list results in the Native mode? or is it all only through the results window?

 

[msiva1981]

I tried with just a simply supported beam with a point load
I decreased the value of point load (hoping that Pro Mechanica was showing me some extreme values)
But did not help.
Here is the details
1. Model 120" long with central load of 200 lbs applied in negative y
2. Section W4x13
3. Results
a. Displacement
Pro Mech 0.02285 in
ANSYS 0.02256 in
b. Max Von mises
Pro Mech 11,200 psi
ANSYS 1197 psi
I do not know what might be wrong
Can someone help me here
Thanks
Siva

 

[Remmerv]

If you did run the MECHANICA analysis you would have noticed the warning message about the load singularity your point-load causes. You should put your load at a surface, eg. by using a surface region around the point. MECHANICA will always find the peak stresses caused by singularities so you will always see that MECHANICA will produce higher peak stresses when singularities are present in the model. Also sharp corners will produce the same effect. You will only see similar results in ANSYS if you increase the number of elements at those locations.


If you put the von Mises plot in the same color legend (and values)in both Ansys and MECHANICA you will see that the results look very similar (at least if you also used the correct mesh in Ansys, as a rule 3 elements over the wallthickness of the beam). Try running the ANSYS analyses again with much more elements and look if stresses increase significantly.


Have you also tried pairing and compressing the beams to their midsurfaces in MECHANICA and run the analysis as a shell model? You will find the deflections to be the same and overall stresses similar to the solid model, only calculated in approx. 6 seconds!


So nothing wrong with the software, differences in stresses are caused by modelling experience (no offence) and interpretation of the results.


Good luck!
Victor

 

[Kaz Z06]

I agree with Victor's comments. There are other ways to solve this type of problem - beams, and shells. In the interest of demonstrating comparative results, I have continued the example in solids. Please find the attached zip files I have included - one for Mechanica files and one for ANSYS. I could not include the ANSYS file as it is too large to upload. Images of results are there as well. I have simplified the model using symmetry and used ANSYS Workbench (v11)instead of "classic" ANSYS. I did not create multiple elements through the web of the beam (which is NOT good practice), but I did turn on mid-sided nodes to help flexibility here. I did move the load to a surface, as Victor also suggested. The results are almost identical from Mechanica to Workbench.Users of ANSYS must be VERY careful with mesh qualityin ANSYS as h element technology is very sensitive to the density and distribution of the mesh and the user must know the difference from a good mesh to a bad mesh. My example still requires more refinement in ANSYS to arrive at a result that would more closely match the Mechanica answer. The model in general requires more detailing of sharp corners as well since these will cause stress concentrations - maybe there are fillets or rounds or welds here to minimize these sharp edges. In summary, Mechanica and ANSYS should agree on all problems both are equipped to handle.


2007-11-02_082112_Mechanica_files.zip


2007-11-02_083317_ANSYS_files.zip


Cheers,


Chris

 

[msiva1981]

Hi all,
Thanks for your replies Victor and Chris. Sorry for responding a little later. I was travelling for the last week and was away from the computer for long. First of all let me tell a little bit about myself. I shall expand on this a little later. Iam a Mechanical Engineer basically into Design using AutoCAD primarily having decent knowledge of Pro E Modelling. . I am just trying to expand my knowledge in Design by venturing into new areas and having worked on Pro E i naturally got in to Pro Mechanica. I had taken some courses in college that taught the basics of FEM (Shape functions, what nodes are? Elements are etc

 

[SlavoM]

Hi,


try to change classical h method to p methodat begining of problem definition under Ansys


After successful solution try to compare results


Ansys can solve linear struct problem with p method of corse...

 

[CaptnPea]

Where do I start to understand the how these programs handle
FEM (what is a good modeling technique?
When to use a dense mesh?
How to benchmark?
What type of solving function to use?
When to use solid elements?
When to use beams and shells?
Any resource, any book

Thanks
Siva

Good modeling tecnique comes with time, every problem is different and likely has a dozen or more good approaches to solving it. So just keep working along and asking qood questions you be an "expert" before you know it. Good judgement is all it takes.


Mesh Size: I don't use H elements currently, but, in the past I would start coarse with the mesh then refine it until I got an exceptable difference between the new model and the previous (depends on what the application is, safty concern etc...). In areas of greater strain differential you want more elements, so focus on refine meshes around corners, load application, boundry conditionsor other stress risers.


Benchmark: Model something you can test, run the test and compare the results the work you model techinque until you get corralation. Start with simple beamsor other structure then start working into contact analysis in built up assemblies. You find it is not really too hard to get dialed in on deflections, stresses and predicting failure is harder. It really depends on what your doing, how accurate you need to be in stresses, in 98% of the work I've done in automotive, and consumer goods deflection ruled the design more than pushing the limits of strength.


Solving function: depends on model, computer, time. In mechanica you can stick with default settings to start, but, do read the help on what the differences are.


Solids: Depends on the part, if not an even thickness (shell) sheetmetal, some plasitc components, use solids. Beams, when your building a truss, or need a quick element to tie solids or shells together.


Read:


Building Better Products with Finite Element Analysis, Vince Adams and Abraham Askenazi. isbn 1-56690-160X


Good book to go with mechanica.

 

[bgervais@drs.ca]

Hi msiva1981,<?:namespace prefix = o ns = "urn:schemas-microsoft-comfficeffice" />


I do not consider myself an analyst but more of a design/analyst (one whouses FEM to design). I used I-DEAS TMG/ESC/NASTRAN/Model Solution for about 7 years and I recently switched to a new company who uses Pro/Mechanica. You are where I was about 8 years ago when I tried using Cosmos/M. Here are a few tips that really helped me get started:


1. Buy a good book that teaches fundamental dos and don't about FEA (not a University type math text book). My favorite is Building Better Products with Finite Elements Analysis (Adams/Askenazi). Without this book I would be lost.


2. Get training on the tool you are using. I know it is a hardfor companies to accept training today however specific tool training is important. Every FEA tool has specific weaknesses and strengths with respect to their solvers. Only a tool specific course will identify these weaknesses and strengths and give you the confidence to use the tool successfully.


3. Understand the types of elements you are using and their limitations. Only use the element types you are comfortable with.


4. Sketch out the way you are going to model the FEM. (Example: a stair casecan be beams for the supports and shells for the steps.) Once you have a clear understanding of the model and how to read it then and only then do you start meshing.(Example: shells will have singularities where the beams connect) Do not just free mesh a solid part for every solve. Garbage=Garbage out.


5. Validate.. Validate.. Validate... Create at least 2 solves with different mesh configurations. (Example: Use all shells and then all solid elements for a plate). If thesolves are close then you areon your way to building your confidence. When they do not match try and figure out why. It could be a number of reasons but do not give up on the issue. After a while you will have enough confidence to avoid validation models on certain problems.


6. Test... There is a lot of pressure from companies to do analysis and eliminate the need for test. In order to build your confidence build prototypes of your models and test them. After a few validation tests you will have the confidence to avoid the tests but let it be your call.





7. Time.. If you are expecting to pick up FEA as fast as you picked Pro/Ethen you should adjust your expectations. Learning Parasolid models takes days maybe weeks. Learning FEA takes years. Do not let this discourage you because once youbecome good at FEAthe rewards are tremendous. Your designs will becomerefined and your company will be able to avoid unnecessary tests and field failures.

 

[msiva1981]

Thank you CaptnPea an bgervais All your information has given me some insight on what i need to be done. I am sure i need a strong understanding of basic concepts of engineering and a good understanding of Dos and Dont's of FEA. To tell you honestly, i was looking for a book to teach me ProMechanica. The ones i found did not help much and Pro Mechanica got me frustated as i was not able to benchmark some of my Thermal problems. I have access to ANSYS also and found a book named FINITE ELEMENT ANALYSIS
Theory and Applications with Ansys By Saeed Moaveni. I am using it at the moment. Seems to be a pretty decent one. I am already on the look out for
" Building Better Products with Finite Element Analysis, Vince Adams and Abraham Askenazi" I stay out of America now. Is there an International edition for this one i could buy. Iam in India. But anyways, Thankyou for all the pointers and help. I feel all i need at the first place is a good book to guide me into the field of FEM
Thanks
Siva